I have a designed a battery charger in simulink and for the sake of completeness and as a learning experience, I would like to explore EMI filtering and design one for it (as a simulation model).

I have started learning about EMI and filter design and started with this video:https://www.youtube.com/watch?v=FwxtnMfrynM

However it suggests that you design the filter AFTER your circuit is ready and you measure the frequencies you need to filter with LISN. However my problem is that I won't be having an actual circuit, I only have a simulink model. These are my questions:

  1. Is this how actual EMI filters are always designed? After the actual circuit is ready?

  2. Is there any other way to find out what frequencies I might need to design the filter for and proceed?

  3. Is there any simulation software that can do EMI simulations so that I can get this information?

  • 2
    \$\begingroup\$ For EMI filter interaction with switching converters, I suggest you take a look at a seminar I taught at an APEC conference in 2017. \$\endgroup\$ Commented Mar 28, 2022 at 5:42
  • 2
    \$\begingroup\$ In these modern days you take into account EMI when designing your circuit and you try and use your simulation tools to perform conducted emissions and susceptibility. \$\endgroup\$
    – Andy aka
    Commented Mar 28, 2022 at 8:59
  • 2
    \$\begingroup\$ Usually we start from a 'stock' recommended filter for a similar application (there are handbook for these) and build it in the first design iteration. Then measure, tune and (if everything else fails) do another designed iteration. Sadly EMC is not easily prototipable since often it's all done by parasitic elements \$\endgroup\$ Commented Mar 28, 2022 at 10:35
  • 2
    \$\begingroup\$ 1. Most often yes. 2. Sure, you can simulate it with parasitics included and get a decent overview of what you will have to deal with. 3. Depends on the frequency. Below 10 MHz, any SPICE with first order parasitics is usually good enough start. The higher you go, the more difficult and you need to do an EM field analysis of the board. It's very complex. \$\endgroup\$
    – winny
    Commented Mar 28, 2022 at 10:59

4 Answers 4


I can only speak to my experience in space applications, but I wouldn’t be surprised if this applies to other industries as well.

Is this how actual EMI filters are always designed ? After the actual circuit is ready?

I’ve seen this done both ways. Sometimes you will find a converter module that you want to use and need to design the EMI filter to work with it. Even as I’ve done this though, I still didn’t test the power supply before designing the EMI filter, I simulated it. If you plan on designing your own converter however, it is almost always better to design the EMI filter as part of the DC/DC converter. You can design and simulate the system as a whole prior to building anything to verify it meets requirements. Although simulations aren’t perfect, you can design with enough margin to be confident it will pass.

Is there any other way to find out what frequencies I might need to design the filter for and proceed?

As SteveSh’s answer says, this depends on your requirements, and your expected conducted emissions. You don’t need to test your power supply to know what those expected emissions are, they can be determined through analysis of the design. Once you know what you have and what you need, you can design something to meet those needs. It’s sometimes an iterative process between changing the converter design and the filter design to get a working solution.

Is there any simulation software that can do EMI simulations so that I can get this information?

You can do conducted emissions simulations in Spice and SIMPLIS. I imagine you can do it in Simulink if you make your model well enough but I’ve never tried that. I’ve also heard of software specifically made for EMI simulations, although I’ve never found the need to try them.

  • 1
    \$\begingroup\$ I liked this better than Steve's response, good as it was, because of how you handled the larger pictures. Appreciated. \$\endgroup\$
    – jonk
    Commented Mar 28, 2022 at 4:26
  • 1
    \$\begingroup\$ > You don’t need to test your power supply to know what those expected emissions are, they can be determined through analysis of the design. How can I go about doing this analysis? Could you suggest any resource where I can read up on this? \$\endgroup\$ Commented Mar 28, 2022 at 8:04
  • 1
    \$\begingroup\$ I don't have access to SPICE or SIMPLIS, is there any other way I can determine conducted emissions? \$\endgroup\$ Commented Mar 28, 2022 at 8:17
  • 3
    \$\begingroup\$ @needbrainscratched Sure you have, LTspice is free and there are other free versions too. \$\endgroup\$
    – winny
    Commented Mar 28, 2022 at 14:15

In answer to you questions as they appear in your post. I am assuming you are asking about conducted emissions (CE) on the input power lines.

  1. No, they are not always designed after the actual circuit is ready. Our power supply group always designs their EMI (input) filters in parallel with the design of the SMPS (Switch Mode Power Supply). To do the filter after the PS is built and tested would add many weeks to the schedule.

And the way you determine what you conducted emissions are is by simulation and modeling.

  1. You need to know what your conducted emissions requirements are, and what the expected conducted emissions you expect from you power supply. Then you can say that "I need a filter with 20 dB of attenuation at 50 kHz", for example. You will actually come up with a curve of attenuation needed vs frequency.

  2. Yes, there are analysis tools that can predict what your conducted emissions will be from your PS. I do not think Simulink is one of them.

Edit 1, Based on OP's Comment

Given what sounds like your tool and/or financial constraints, your only option may be to build and measure.

But that brings up the question of how are you are going to make those CE measurements. Are you going to make them yourself (tricky to do right); contract out to an EMC lab (costly); some other approach?

  • 1
    \$\begingroup\$ Can you suggest any of these analysis/simulation tools that might be free? \$\endgroup\$ Commented Mar 28, 2022 at 8:18
  • 2
    \$\begingroup\$ I do not not know of any that are free. Some of the free or low-cost tools like Spice may be able to analyze parts of the circuit. I may be wrong, but I do no think they have the capability to model the "flow" of switching transients all the way back to the input. \$\endgroup\$
    – SteveSh
    Commented Mar 28, 2022 at 10:23

The best EMI filter is the one that you don't need. So you'd typically start by running the circuit in SPICE, and add parasitic properties of key elements. E.g. decoupling capacitors have ESR and ESL (equivalent series resistance and inductance, respectively). That way, the AC current flowing from the power source is more realistic. And so you know exactly what frequencies are there. Next, your goal is to make those AC currents flow inside your circuit and not reach the power supply, the outputs, the external connections, etc. The first step will be to arrange circuit impedances such that most of the AC current flows in small loops. Some of it will inevitably escape due to nonidealities of components and layout, and that's the part that the EMI filter would deal with.

The approximate process would be as below, and some groups of steps have to be iteratively repeated.

  1. Design the basic circuit and get it to work in SPICE at least.

  2. Choose actual components (real part numbers).

  3. Use the component data sheets and/or characterize the components using a network analyzer to obtain their accurate simulation models that include parasitics.

  4. Substitute equivalent networks of real, non-ideal components for the ideal components in the SPICE model.

  5. Identify the AC current loops of concern in the SPICE model.

  6. Lay out the circuit taking critical current loops into account.

  7. Use an electromagnetic simulator - this could be your head, with enough experience - to approximate the parasitics of the layout.

  8. Add the layout parasitics to the SPICE model.

  9. Re-run the simulation and observe the AC currents flowing from the power source, flowing to the output, flowing to the I/O ports, etc.

  10. Do various things to constrain those currents to flow within your circuit only. The EMI filter is the last line of defense that will do that.

Notice how we haven't actually put anything physically together yet. If your simulations are accurate, as soon as you assemble the prototype, it should work and pass EMC testing at least in respect to conducted emissions - since you were simulating all that.

The simulation model may have some infidelities, which you would now identify by comparing the performance of the prototype with that of the model, and adjust the model to more accurately represent the real circuit. Then the simulation will inform you what changes (if any) are needed to the EMI filter to get things to pass.

It is generally a tall order to use external filters to work around deficiencies of a badly designed circuit. And, unfortunately, the majority of little "switching converter" boards sold for the hobby market are quite atrocious in terms of EMC - precisely because nobody tried to make them behave just by themselves, without external filters. This is a real problem in low-level circuits that are noise-sensitive: with a few "handy" buck/boost/charger boards on the breadboard, you get an intractable mess that takes real effort to clean up in terms of EMC needed just to get it functional - that's even before you begin to think about any other EMC testing.

Some people would argue, and rightly so, that EMC is part of the functionality of the circuit. Thus there's no "make it work" separate from "make it pass EMC testing": it's all part of the same process, and the first prototype should at least have first-order effects taken care of with EMC in mind.


You can just do in models, what you would have done in real life.

Make a model of the LISN (with test points) and attach it to your Simulink model. You would then be able to see what the test points measure in simulation.

As a first pass you would see what conducted emissions you have using idealized components. At that point add filtering to fix any problems that simulation shows.

To make things more accurate you might try adding reasonable values for the parasitic capacitances and inductances on your circuit elements. One way to do that would be to search on some distributor websites (Digikey, Mouser, Avnet, Arrow, Newark, etc) for some real components that are close to what you used in your model. You could then get that information from either a SPICE model (if available) or the datasheets.

It should be noted that without a physical layout, it's probably impossible to figure out what the radiated emission levels would be. You might however be able to determine at what frequencies radiation is likely to occur (typically multiples of the switching frequency, or the ringing frequencies of parasitic elements).


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.